Cost of computing k-kl-omega

I shall analyse low-Re flow over a streamlined 3D body (velomobile at 10 m/s). For this specific task I have been recommended k-kl-omega as suitable model since the problem involves laminar-turbulence transitions where this new model seems to excel.

Q1: Will k-kl-omega work fine for this problem or should I consider simpler models as well? I plan on using Caedium and the target is to dial in on a practical and cost efficient body as part of a master thesis.

I have the impression K-kl-omega need very fine mesh - found a suggestion for 0.3mm boundary cells with 1.15 growth per layer for the 30mm near moving body. I assume that this fine mesh also will require a timestep small enough to let a particle move not more than one cell during a time step. That would require a time step of 0.3 mm / 10 000 mm / s = 30 uS.

Q2: Is the timestep too small?

Assuming Velomobile is 800 mm wide, 1000 mm high and 2500 mm long I plan on making a mesh of approx 6-12 million cells consisting of a rectangular box - "wind tunnel" - LxWxH of 5.0 m x 2.4 m x 2.0 m

Q3: Will the massive computational task simply be overwhelming for a single CPU - quad core with plenty RAM - to be able to converge within 8-16 hours?

I'd like to think that the k-kl-omega turbulence model should be up to the application you describe. However, I would suggest you also consider the default wall function turbulence model (fully turbulent, k-omega SST) and a laminar case. That way you should have a lower bounds (laminar) and upper bounds (fully turbulent) on your drag values.

In terms of the wall spacing for the k-kl-omega model you are looking for a y+ ~=1, whereas for the default wall function turbulence models you should aim for y+ ~=30-300. y+ is dependent on your model and the flow conditions. Pointwise have an online y+ calculator that can estimate the first cell height for a given y+ value.

To efficiently achieve y+ ~=1, you most likely will need high-aspect ratio (stretched) cells. Currently Caedium can not generate such cells, unless you construct a special multiblock volume structure around your model to create a hexahedral mesh. An alternative is to use a 3rd party mesh generator, such as Pointwise.

Given you have a streamlined shape I would suggest you try running a steady-state simulation (always worth a try for any simulation), it will be much faster than running a transient simulation, in which case the time step is irrelevant. For more on steady-state vs transient see "Steady-State or Unsteady CFD Simulation?"

If you are not constrained to match the 'wind tunnel' dimensions then I would suggest you use a half model (assuming symmetry) and ensure that the outer boundary dimensions are at least 5 body lengths away in all directions (in undisturbed air), i.e., LxWxH (m) ~= (7.5 upstream + 15 downstream) x 3 (assuming half model) x 6. For an example see "Flow Over a Rotating Wheel with Moving Ground".

It is a good idea to try different outer boundary distances to ensure that they are not having a significant impact on your results.

For larger cases a quad core CPU will run nearly 4 times faster than a single CPU. A single CPU will not be overwhelmed with a large case, it will just run a lot slower. If your cases are going to be up to 12 million cells then you will require at least 12 GB RAM - otherwise you will see swapping to disk and that will make your simulation run 100 times slower even with a quad core CPU.